CNC Processing School: How Metal Cutting Actually Works

• 1
  What a CNC processing school teaches first: the chip
• 2
  Why a rigid setup matters more than spindle speed
• 3
  How toolpath strategy changes what the part can be
• 4
  What material choice does to the cut
• 5
  Where each CNC process stops being economical

Every CNC operation removes material with a wedge-shaped edge. The tool pushes into the workpiece, the material ahead of the edge shears off, and a chip slides up the rake face. That chip carries most of the heat away. If the chip is thin and powdery, heat stays in the tool and the workpiece. If it is thick and curls cleanly, the cut is running where it should. Reading the chip is the fastest diagnostic on the floor.

Chip load is the thickness of material each cutting edge removes per revolution. On a 12 mm three-flute carbide end mill at 8,000 rpm and 1,200 mm/min feed, the chip load is about 0.05 mm per tooth. Push it to 0.15 mm and the edge may chip. Drop it to 0.01 mm and the tool rubs instead of cutting, which work-hardens stainless and burns the edge. The window is narrower than most CAD models suggest.

The same physics applies to turning. On a Ø50 mm 304 stainless shaft at 180 °C cutting temperature, a 0.2 mm depth of cut with 0.15 mm/rev feed produces a continuous chip that breaks on the insert breaker. A 0.02 mm/rev feed produces a stringy chip that wraps the tool and scratches the finish. Feed rate is not a comfort setting. It is the variable that decides whether the insert survives the pass.

Hardness sets the ceiling. Aluminium 6061 machines at 300–600 m/min surface speed with HSS or carbide. Titanium Ti-6Al-4V runs at 30–60 m/min and needs flood coolant because the chip conducts heat poorly. Inconel drops to 20–40 m/min and often requires ceramic or coated carbide. The same program that cuts aluminium in two minutes will destroy a tool in titanium in ten seconds if the speeds are not changed.

• 1
  Chip colorSilver to straw is normal on steel. Blue or black means the edge is too hot.
• 2
  Chip shapeShort curls are healthy. Long strings mean feed is too low.
• 3
  Chip thicknessAim for 0.03–0.12 mm per tooth on carbide in steel.
• 4
  CoolantFlood on titanium and stainless; air blast on aluminium and plastics.

A CNC machine is a spring. The tool, holder, spindle, column and fixture all bend under cutting force. A 12 mm carbide end mill with 60 mm of stickout deflects roughly 0.03 mm under a 500 N side load. Shorten the stickout to 30 mm and the same load deflects about 0.004 mm. That difference decides whether a ±0.05 mm slot holds tolerance. The machine itself rarely limits the cut. The tool assembly does.

Chatter is the visible symptom of that spring. It appears as a wavy pattern on the wall and a high-pitched sound. The fix is not always slower speed. Often it is a shorter tool, a stiffer holder, or a change in the tooth passing frequency so the tool does not excite the natural frequency of the setup. On deep pockets, a 4 mm tool at 4× diameter depth needs a 6 mm shank or a shrink-fit holder to stay quiet.

Fixturing multiplies the problem. A part held in a vise with 20 mm of jaw contact behaves differently from the same part held in a custom soft jaw with full-length contact. Thin walls move away from the cutter. Long parts sag in the middle. For a 4,000 mm part, the table supports the weight, but the middle still deflects under its own mass. Support every span longer than 8× its thickness.

Thermal growth is the slow error. Aluminium expands about 23 μm per metre per degree Celsius. A 300 mm aluminium part warming 5 °C from cutting grows 0.035 mm. On a ±0.005 mm job, that is seven times the tolerance. Coolant, a temperature-controlled shop, and finishing passes with light depth of cut keep the part near 20 °C. Measure after the part settles, not while it is hot.

• 1
  Stickout ruleKeep tool length under 4× diameter for finishing.
• 2
  Wall thicknessBelow 1.5 mm, expect to add a finishing pass.
• 3
  Clamp positionClamp directly over the cutting zone when possible.
• 4
  Thermal driftLet parts cool 10–20 minutes before final inspection.

A CNC processing school spends as much time on toolpath as on the machine. A square internal corner cannot be cut by a round tool. If a drawing shows a 90° pocket corner, the tool leaves a radius equal to its own radius. A 6 mm end mill leaves a 3 mm radius. Designers who want a sharp corner must either accept the radius, add a relief, or specify EDM, which is a different process with a different cost.

Depth-to-diameter ratio sets the number of passes. A 10 mm tool cutting a 40 mm deep pocket needs four passes at 1× diameter, or two passes at 2× diameter with a high-feed path. High-feed toolpaths tilt the tool and take a shallow radial cut at high feed. They remove material faster and put less radial load on the tool. The trade-off is more program lines and more machine time on complex surfaces.

Five-axis motion solves reach, not tolerance. A simultaneous 5-axis center with a Ø400 mm rotary table can machine an impeller or a medical implant in one setup. That single setup removes the stacked error of four separate fixtures. But the machine cannot fix a bad datum. If the first operation establishes the datum from a rough surface, every later operation inherits that error. Pick a machined face, a bore, or a ground pad as the primary datum.

Thin floors and tall ribs behave differently from solid blocks. A 0.5 mm floor on a 50 mm pocket will vibrate unless the toolpath stays in constant contact with the material. Trochoidal paths and adaptive clearing keep the radial engagement constant, which keeps the force constant, which keeps the deflection constant. That is the real reason those paths exist: not speed, but predictable force.

• 1
  Internal cornerMinimum radius equals tool radius; call it out on the print.
• 2
  Pocket depthKeep under 4× tool diameter per setup when possible.
• 3
  Datum choiceUse a machined face, never a cast or rough surface.
• 4
  Adaptive clearingBest for deep pockets, thin floors and hard alloys.

Aluminium 6061-T6 is the default for prototypes because it cuts fast and holds ±0.005 mm without drama. It also scratches and dents easily. 7075 is stronger but gummier; it needs sharper tools and more coolant. 2024 machines well but corrodes fast, so it usually gets anodizing within a day of cutting. The material data sheet does not tell you any of this. The chip does.

Stainless 303 is the free-machining grade and the easiest to turn. 304 and 316 work-harden if the tool rubs, so feeds must stay high and depths must stay above the work-hardened layer. 17-4PH in the H900 condition cuts like a tool steel and needs carbide with a hard coating. The condition matters more than the alloy name. A 316 part in the annealed state and the same part in the cold-worked state behave like two different materials.

Titanium and Inconel are heat problems, not hardness problems. Ti-6Al-4V conducts heat slowly, so the edge reaches 600 °C while the part stays cool. High-pressure coolant through the tool is the standard answer. Inconel 718 at 45 HRC needs ceramic inserts or coated carbide at low speed and heavy feed to get under the work-hardened skin. Neither metal rewards a light finishing pass.

Surface finish follows the same logic. A Ra 0.8–1.6 μm finish is a normal machined result. Ra 0.2–0.8 μm needs a finishing pass at low feed and a sharp tool, and it may need polishing after. Bead blasting hides tool marks but does not improve dimensional accuracy. Anodizing adds 5–25 μm of oxide, which changes a press fit. Specify the finish before the tolerance, not after.

• 1
  Aluminium6061, 7075, 2024, 6082, 5052; anodize soon after cutting.
• 2
  Stainless303 for ease, 304/316 for corrosion, 17-4PH for strength.
• 3
  TitaniumTi-6Al-4V needs through-tool coolant and low surface speed.
• 4
  FinishRa 0.8–1.6 μm standard; Ra 0.2–0.8 μm on request.